Last changed 2005-May-1
The physical design of the printed circuit board involves two major steps: parts placement and trace routing. The Mentor tool used for these steps is called Layout. In the command window where you were running Design Architect (you did exit it, didn't you?), start Layout by typing:
hoodoo:/home/stirra/classes/engr357/pcbtut> run_en2k layout osc1
You should try to put all of your components and traces on the top surface of the circuit board, as you will only have etched traces on the top side, and any jumpers or components on the back side will require holes drilled through the board for connections.
The place components icon gets you to the palette that is used for position all your parts on your board. Since many components look alike, I recommend using place components by reference to position them systematically from your schematic. While the part is being placed, you can rotate it in 90 degree increments by doing shift-right-click, or flip it to the back side of the board (only for smd parts on double sided PCB's!) with ctrl-right-click. Fix the part with a left-click.
When you have placed all the parts on the circuit board in your desired pattern, you are ready to route traces. The tool constrains you to connecting pads in the exact topology specified in your schematic. If you change your mind on your circuit, you have to go back to Design Architect to change your schematic before continuing with layout.
Analog circuits are best routed by hand, and power and ground traces for complex digital circuits should also be manually routed. The rest of a complex digital circuit may be autorouted. Autorouting will be discussed at the end of this tutorial.
Use the Route icon to bring up the route palette. Before starting any routing, use the "Setup Routing" icon to be sure the current setup is satisfactory. The via selected should be small (v026 for a 0.026in diameter hole works well), and the trace width should be set to your desired default value (starts out as 0.015").
Click on "Route Interactive" to begin routing a trace. Click left on a guide (thin green line) to start routing. Click again for each turn you wish to make in the trace. When you get your trace to the destination pad (or a previously routed trace segment), the trace will be completed when you left-click. You may reroute a trace with the same method, and you can delete a trace segment by selecting it and hitting "Del". Frequently you may wish to change the width of a trace (power or ground traces, for example). The easiest way to do this is to select the trace you wish to modify, and type "$change_trace_width(0.02)" (to get a 0.020" width for example) with the cursor anywhere in the main window. As soon as you start typing a little text window will pop up. When you hit return your trace will have a new width (provided no clearance rules were violated).
You may wish to change (or remove) the text identifying the board name and the layers. Click on the red "Text" icon to bring up the text palette. To change text select your text and click on the "Change Text" icon.
Frequently you will have large areas of your board that are empty. To extend the life of the copper etchant, it is helpful to fill the empty areas with copper after your traces are all finished. Do this by going to the Area Fill palette. Click on "Add Fill" and select the four corners of the board. A double-click on the last corner will complete the fill.
To switch into the AutoActive autorouter, click on the red BoardStationRE icon in the upper right of the Layout screen. Layout will be iconified, and a minute or so later the AutoActive window will appear. Before you can start the autorouting process, you have to request the license from the Setup menu. After obtaining the license, you can choose Route -> Autoroute, and then click on Route in the Auto Route dialog box. The default parameters in the dialog box should be sufficient for most designs. If the autorouter is not successful at routing your design to 100% completion, you will likely need to move some of the parts to alleviate congested areas of the board. You can move parts while in AutoActive (use the Place menu), or you can return to Layout (use File -> Return to BoardStation) and do your placement there.
When you are finished with autorouting, choose File -> Return to BoardStation and be sure to check "Yes" for each of the "save" questions asked. You will then be returned to Layout.
When you are finished with your board, or if you need to make a schematic change in DA, just select MGC->Exit. Be sure you select "Save Design" and "Backannotate"! Failure to do either of these will cause you to lose your work. You can do intermediate saves with File->Save->Design All and File->Back Annotate.
